Siemens SINUMERIK 802D sl Programming Manual page 141

04.07
Programming in the cylindrical interpolation mode
In the cylindrical interpolation mode, only the following G codes can be used: G00,
G01, G02, G03, G04, G40, G41, G42, G65, G66, G67, G90, G91, and G7.1. Con-
cerning the G00 command, only the axes not included in the cylindrical plane can
be designated in the G00 mode.
1. G00 (positioning command)
The G00 command can be specified only for the axes which are not included in
the cylindrical plane. Positioning is not possible on the cylindrical plane. If posi-
tioning is required for the axis which is included in the cylindrical plane, the cy-
lindrical interpolation mode must be canceled once.
2. G01 (linear interpolation command)
This command can be specified for all axes. However, it is not allowed to speci-
fy the axis included in the cylindrical plane and the one not included in the cylin-
drical plane in the same block.
The designation of the end point for the linear interpolation should be made in
either "mm" or "inch" for both the linear and rotary axes.
Feedrates of the axes are controlled so that the vector sum (tangential velocity
in the direction of tool movement) of the linear axis feedrate and the rotary axis
feedrate will be the feedrate specified in the program.
3. G02/G03 (circular interpolation commands)
The circular interpolation commands can be specified only for the axes included
in the cylindrical plane.
The designation of the end point for the circular interpolation should be made in
either "mm" or "inch" for both the linear and rotary axes.
The radius for the circular interpolation should be specified by an R command
or by specifying the center of the arc. When an R command is used, designa-
tion of the radius should be made in either "mm" or "inch". If the center of the
arc should be designated instead of the R command, specify the distance from
the start point to the center of the arc by signed incremental value using ad-
dresses I, J, and K.
S If the linear axis is X-axis, use I and J assuming the XY plane.
S If the linear axis is Y-axis, use J and K assuming the YZ plane.
S If the linear axis is Z-axis, use K and I assuming the ZX plane.
4. G40/G41/G42
The tool radius offset C function can be used only in the cylindrical plane. The
D command specifying the offset memory number may be specified in any
block. To execute tool radius offset in the cylindrical plane, turn ON the cylindri-
cal interpolation mode and the tool radius offset mode.
The tool path in the cylindrical plane is offset by the tool radius set in the tool
offset data memory. The direction of offset is specified by G41 and G42.
It is necessary to cancel the offset by specifying the G40 command before turn-
ing the cylindrical interpolation mode OFF.
5. G90/G91 (absolute/incremental commands)
It is allowed to change the dimension data designation mode between absolute
and incremental while in the cylindrical interpolation mode. Designation can be
made in the same manner as in the normal mode.
© Siemens AG 2007 All rights reserved
SINUMERIK 802D sl/840D/840D sl/840Di/840Di sl/810D ISO Milling (PGM) -- 04.07 Edition
Enhanced Level Commands
4.7 Cylindrical interpolation (G07.1)
4-141